*GET

*GET, Par, Entity, ENTNUM, Item1, IT1NUM, Item2, IT2NUM
Retrieves a value and stores it as a scalar parameter or part of an array parameter.

APDL: Parameters

Par: The name of the resulting parameter. See *SET for name restrictions.
Entity: Entity keyword. Valid keywords are NODE, ELEM, KP, LINE, AREA, VOLU, etc., as shown for Entity = in the tables below.
ENTNUM: The number or label for the entity (as shown for ENTNUM = in the tables below). In some cases, a zero (or blank) ENTNUM represents all entities of the set.
Item1: The name of a particular item for the given entity. Valid items are as shown in the Item1 columns of the tables below.
IT1NUM: The number (or label) for the specified Item1 (if any). Valid IT1NUM values are as shown in the IT1NUM columns of the tables below. Some Item1 labels do not require an IT1NUM value.
Item2, IT2NUM: A second set of item labels and numbers to further qualify the item for which data are to be retrieved. Most items do not require this level of information.

Notes

*GET retrieves a value for a specified item and stores the value as a scalar parameter, or as a value in a user-named array parameter. An item is identified by various keyword, label, and number combinations. Usage is similar to the *SET command except that the parameter values are retrieved from previously input or calculated results.

Example 8: *GET Usage

*GET,A,ELEM,5,CENT,X returns the centroid x location of element 5 and stores the result as parameter A.

*GET command operations, and corresponding get functions, return values in the active coordinate system (CSYS for input data or RSYS for results data) unless stated otherwise.

A get function is an alternative in-line function that can be used instead of the *GET command to retrieve a value. For more information, see Using In-line Get Functions in the Ansys Parametric Design Language Guide.

Both *GET and *VGET retrieve information from the active data stored in memory. The database is often the source, and sometimes the information is retrieved from common memory blocks that the program uses to manipulate information. Although POST1 and POST26 operations use a *.rst file, *GET data is accessed from the database or from the common blocks. Get operations do not access the *.rst file directly. For repeated gets of sequential items, such as from a series of elements, see the *VGET command.

Most items are stored in the database after they are calculated and are available anytime thereafter. Items are grouped according to where they are usually first defined or calculated. Preprocessing data will often not reflect the calculated values generated from section data. Do not use *GET to obtain data from elements that use calculated section data, such as beams or shells.

When the value retrieved by *GET is a component name, the resulting character parameter is limited to 32 characters. If the component name is longer than 32 characters, the remaining characters are ignored.

Most of the general items listed below are available from all modules. Each of the sections for accessing *GET parameters are shown in the following order:

The *GET command is valid in any processor.

General Items

*GET General Entity Items

Table 115: *GET General Items, Entity = ACTIVE

`Entity` = ACTIVE, `ENTNUM` = 0 (or blank)
GET, Par, ACTIVE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
INT		Current interactive key: 0=off, 2=on.
IMME		Current immediate key: 0=off, 1=on.
MENU		Current menu key: 0=off, 1=on.
PRKEY		Printout suppression status: 0=/NOPR, 1=/GOPR or /GO
UNITS		Units specified by /UNITS command: 0 = USER, 1 = SI, 2 = CGS, 3 = BFT, 4 = BIN, 5 = MKS, 6 = MPA, 7 = uMKS.
ROUT		Current routine: 0 = Begin level, 17 = PREP7, 21 = SOLUTION, 31 = POST1, 36 = POST26, 52 = AUX2, 53 = AUX3, 62 = AUX12, 65 = AUX15.
TIME	WALL,CPU	Current wall clock or CPU time. Current wall clock will continue to accumulate during a run and is not reset to zero at midnight.
DBASE	LDATE	Date of first modification of any database quantity required for POST1 operation. The parameter returned is `Par` = YEAR10000 + MONTH100 + DAY.
DBASE	LTIME	Time of last modification of any database quantity required for POST1 operation. The parameter returned is `Par` = HOURS10000 + MINUTES100 + SECONDS.
REV		Minor release revision number (5.6, 5.7, 6.0 etc.). Letter notation (for example, 5.0A) is not included.
TITLE	0,1,2,3,4	Item2: START IT2NUM: `N` Current title string of the main title (`IT1NUM`=0 or blank) or subtitle 1, 2, 3, or 4 (`IT1NUM`=1,2,3, or 4). A character parameter of up to 8 characters, starting at position `N`, is returned.
JOBNAM		Item2: START IT2NUM:`N` Current Jobname. A character parameter of up to 8 characters, starting at position `N`, is returned. Use DIM and DO to get all 32 characters.
PLATFORM		The current platform.
NPROC	CURR, MAX, MAXP	The number of processors being used for the current session, or the maximum total number of processors (physical and virtual) available on the machine, or the maximum number of physical processors available on the machine. This only applies to shared-memory parallelism.
NUMCPU		Number of distributed processes being used (distributed-memory parallel solution).

Table 116: *GET General Items, Entity = CMD

`Entity` = CMD, `ENTNUM` = 0 (or blank) The following items are valid for all commands except star (*) commands and non-graphics slash (/) commands.
GET, `Par`, CMD, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
STAT		Status of previous command: 0=found, 1=not found (unknown).
NARGS		Field number of last nonblank field on the previous command.
FIELD	2,3...`N`	Numerical value of the `N`th field on the previous command. Field 1 is the command name (not available)

Table 117: *GET General Items, Entity = COMP

`Entity` = COMP, `ENTNUM` = 0 (or blank)
GET, `Par`, COMP, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NCOMP		Total number of components and assemblies currently defined.

`Entity` = COMP, `ENTNUM` = `n` (`n`th component)
GET, `Par`, COMP, `n`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NAME		Name of the `N`th item (component or assembly) in the list of components and assemblies. A character parameter is returned.

`Entity` = COMP, `ENTNUM` = `Cname` (component or assembly name)
GET, `Par`, COMP, `Cname`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Type of component `Cname:` 1=Nodes, 2=Elements, 6=Keypoints, 7=Lines, 8=Areas, 9=Volumes, 11-15=Subcomponents (11=subcomponent at level 1, 12=subcomponent at level 2, etc.).
NSCOMP		Number of subcomponents (for assemblies).
SNAME	`N`	Name of `N`th subcomponent of assembly `Cname`. A character parameter is returned.

Table 118: *GET General Items, Entity = GRAPH

`Entity` =GRAPH, `ENTNUM` = N (window number)
GET, `Par`, GRAPH, N, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ACTIVE		/WINDOW status: 0=off, 1=on.
ANGLE		/ANGLE `THETA` angle.
CONTOUR	`Name`	/CONTOUR value for `Name`, where `Name` = VMIN, VINC, or NCONT.
DIST		/DIST `DVAL` value.
DSCALE	DMULT	/DSCALE `DMULT` value.
EDGE		/EDGE `KEY` value.
FOCUS	X, Y, Z	/FOCUS `CIN`, `YF`, or `ZF` value.
GLINE		/GLINE `STYLE` value.
MODE		/USER or /AUTO setting: 0=user, 1=auto.
NORMAL		/NORMAL `KEY` value.
RANGE	XMIN, XMAX, YMIN, YMAX	/WINDOW `XMIN`, `XMAX`, `YMIN` , or `YMAX` screen coordinates.
RATIO	X, Y	/RATIO `RATOX` or `RATOY`value.
SSCALE	SMULT	/SSCALE `SMULT` value.
TYPE		/TYPE `Type` value.
VCONE	ANGLE	/VCONE `PHI` angle.
VIEW	X, Y, Z	/VIEW `XV`, `YV`, or `ZV` value.
VSCALE	VRATIO	/VSCALE `VRATIO` value.

`Entity` =GRAPH, `ENTNUM` = 0 (or blank)
GET, `Par`, GRAPH, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
DISPLAY		/SHOW `VECT` setting: 0=raster, 1=vector.
ERASE		/ERASE or /NOERASE setting: 0=no erase, 1=erase.
NDIST		Largest nodal range for current model (DX, DY, or DZ of the model).
NUMBER		/NUMBER `NKEY` value.
PLOPTS	`Name`	/PLOPTS setting of `Name`, where `Name`=LEG1, LEG2, LEG3, INFO, FRAM, TITL, MINM, or VERS.
SEG		Segment capability of graphics driver: 0=no segments available, 1=erasable segments available, 2=non-erasable segments available.
SHRINK		/SHRINK `RATIO` value.

Table 119: *GET General Items, Entity = PARM

`Entity` = PARM, `ENTNUM` = 0 (or blank)
GET, `Par`, PARM, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
MAX		Total number of parameters currently defined.
BASIC		Number of scalar parameters (excluding parameters beginning with an underscore _, array parameters, and character parameters).
LOC	`Num`	Name of the parameter at the `Num` location in the parameter table. A character parameter is returned.

`Entity` = PARM, `ENTNUM` = Name (parameter name)
GET, `Par`, PARM, `Name`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Parameter type: 0 = scalar, 1 = array, 2 = table, 3 = character scalar, 4 = character array, -1 = undefined
DIM	X(1), Y(2), Z(3), (4), (5)	Row (X or 1), Column (Y or 2), Plane (Z or 3), Book (4), or Shelf (5) dimension of array parameter.
CSYS		Local coordinate system number
VAR	1, 2, 3, 4, 5	Name of primary variables 1-5. Primary variable names are character strings.
If Item1 = DIM and ITNUM refers to a dimension that does not exist, the program assigns a value of -1 to `Par`. If Item1 = CSYS and no local coordinate system number was assigned to the array parameter (`Name`), the program assigns a value of ZERO to `Par`. If Item1 = VAR and if IT1NUM refers to a primary variable that does not exist, the program assigns a blank value to `Par`.

Table 120: *GET General Items, Entity = TBTYPE

`Entity` = `TBTYPE` , `ENTNUM` = `MatID` (where TBTYPE is the material table type as defined via the TB command, such (ELASTIC, CTE, etc.), and `MatID` is the material ID) Evaluates a material property coefficient for a given set of input field variables.
GET, `Par`, `TBTYPE`, `MatID`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`, `Fld1`, `Fld2`*,...
Item1	IT1NUM	Description
TBEV: Material table evaluation for query at a given field variable	`SINDEX` = Subtable index (1 - max number of subtables)	Item2: `CINDEX` = Coefficient index
		IT2NUM: `N` = Number of field variables input
		`Fld1`, `Fld2`, . . . , : `Val` = Value of the field variable(s), entered in the same order specified via the TBFIELD command(s)

Preprocessing Items

*GET Preprocessing Entity Items

Table 121: *GET Preprocessing Items, Entity = ACTIVE

`Entity` = ACTIVE, `ENTNUM` = 0 (or blank)
GET, `Par`, ACTIVE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
SEG		Segment capability of graphics driver: 0=no segments available, 1=erasable segments available, 2=non-erasable segments available.
CSYS		Active coordinate system.
DSYS		Active display coordinate system.
MAT		Active material.
TYPE		Active element type.
REAL		Active real constant set.
ESYS		Active element coordinate system.
SECT		Active section.
CP		Maximum coupled node set number in the model (includes merged and deleted sets until compressed out).
CE		Maximum constraint equation set number in the model (includes merged and deleted sets until compressed out).

Table 122: *GET Preprocessing items, Entity = AREA

`Entity` = AREA, `ENTNUM` = `N` (area number)
GET, `Par`, AREA, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ATTR	`Name`	Number assigned to the attribute, `Name`, where `Name`=MAT, TYPE, REAL, ESYS, KB,KE,SECN, NNOD, NELM, or ESIZ. (NNOD=number of nodes, NELM=number of elements, ESIZ=element size.)
ASEL		Select status of area `N`: -1=unselected, 0=undefined, 1=selected. Alternative get function: ASEL(`N`).
NXTH		Next higher area number above `N` in selected set (or zero if none found).
NXTL		Next lower area number below `N` in selected set (or zero if none found).
AREA		Area of area `N`. (ASUM or GSUM must have been performed sometime previously with at least this area `N` selected).
LOOP	1,2,...,`I`	`Item2`: LINE, `IT2NUM`: 1,2,...,`p` Line number of position `p` of loop `I`

`Entity` = AREA, `ENTNUM` = 0 (or blank)
GET, `Par`, AREA, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX, MIN	Highest or lowest area number in the selected set.
NUM	MAXD, MIND	Highest or lowest area number defined.
COUNT		Number of areas in the selected set.
AREA		Combined areas (from last ASUM or GSUM).
VOLU		Combined volume of areas (from last ASUM or GSUM. For 3D area elements, thickness is determined from area attributes (AATT). For 2D elements, area attributes are ignored and unit thickness is assumed.
CENT	X, Y, Z	Centroid X, Y, or Z location of areas (from last ASUM or GSUM).
IOR	X, Y, Z, XY, YZ, ZX	Moments of inertia about origin (from last ASUM or GSUM).
IMC	X, Y, Z, XY, YZ, ZX	Moments of inertia about mass centroid (from last ASUM or GSUM).
IPR	X, Y, Z	Principal moments of inertia (from last ASUM or GSUM).
IXV	X, Y, Z	Principal orientation X vector components (from last ASUM or GSUM).
IYV	X, Y, Z	Principal orientation Y vector components (from last ASUM or GSUM).
IZV	X, Y, Z	Principal orientation Z vector components (from last ASUM or GSUM).

Table 123: *GET Preprocessing Items, Entity = AXIS

`Entity` = AXIS, `ENTNUM` = 0 (or blank)
GET, `Par`, AXIS, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT	--	Number of defined sections.
NUM	MAX	Largest section number defined.

`Entity` = AXIS, `ENTNUM` = `ID` (axis section identifier)
GET, `Par`, AXIS, `ID`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE	--	Section type, for `ID` -- SECTYPE command (always AXIS for axis sections).
NAME	--	Name defined for the given section ID number.
DATA	`nnn`	Where `nnn` is the location in the SECDATA command for the given section ID number.

Table 124: *GET Preprocessing Items, Entity = CDSY

`Entity` = CDSY, `ENTNUM` = `N` (coordinate system number)
GET, `Par`, CDSY, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
LOC	X, Y, Z	X, Y, or Z origin location in global Cartesian system.
ANG	XY, YZ, ZX	THXY, THYZ, or THZX rotation angle (in degrees) relative to the global Cartesian coordinate system.
ATTR	`Name`	Number assigned to `Name`, where `Name`=KCS, KTHET, KPHI, PAR1, or PAR2. The value -1.0 is returned for KCS if the coordinate system is undefined.
NUM	MAX	The maximum coordinate system number

Table 125: *GET Preprocessing Items, Entity = CE

`Entity` = CE, `ENTNUM` = `N` (constraint equation set)
GET, `Par`, CE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
If N = 0, then
MAX		Maximum constraint equation number
NUM		Number of constraint equations
If N > 0, then
NTERM		Number of terms in this constraint equation
CONST		Constant term for this constraint equation
TERM	number	Item2 = NODE: Gives the node for this position in the constraint equation. Item2 = DOF: Gives the DOF number for this position in the constraint equation. (1–UX, 2–UY, 3–UZ, 4–ROTX, etc.) Item2 = COEF: Gives the coefficient for this position in the constraint equation.

Table 126: *GET Preprocessing Items, Entity = CMPB

Entity = CMPB, ENTNUM = N (composite beam section identification number)

*GET, Par, CMPB, N, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

COUNT Number of defined sections. If Item1 = COUNT, then N is blank.

NUM MAX Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS Returns a 1 if the section exists and if it is a CMPB section.

NAME The 8-character section name defined via the SECTYPE command.

One of the following:

CBMX

CBTE

CBMD

Item2 = NTEM (the number of temperatures for CBMX, CBTE, or CBMD data).

One of the following:

CBMX

CBTE

CBMD

Item2 = TVAL; IT2NUM = nnn

where nnn is the temperature value (< = NTEM).

One of the following:

CBMX

CBTE

CBMD

nnn

Item2 = TEMP; IT2NUM = tval

Where nnn is the location in the CBMX, CBTE, or CBMD command for the given coefficient number, and tval is the temperature value.

Table 127: *GET Preprocessing Items, Entity = CP

`Entity` = CP, `ENTNUM` = `N` (coupled node set)
GET, `Par`, CP, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
If N = 0, then
MAX		Maximum coupled set number
NUM		Number of coupled sets
If N > 0, then
DOF		The degree of freedom for this set (1–UX, 2–UY, 3–UZ, 4–ROTX, etc.)
NTERM		Number of nodes in this set.
TERM	number	Item2 = NODE: Gives the node for this position number in the coupled set.

Table 128: *GET Preprocessing Items, Entity = CSEC

`Entity` = CSEC, `ENTNUM` = 0 (or blank)
GET, `Par`, CSEC, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT	--	Number of defined sections.
NUM	MAX	Largest section number defined.

`Entity` = CSEC, `ENTNUM` = `ID` (contact section identifier)
GET, `Par`, CSEC, `ID`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE	--	Section type, for `ID` -- SECTYPE command (always CONT for contact sections).
NAME	--	Name defined for the given section ID number.
DATA	`nnn`	Where `nnn` is the location in the SECDATA command for the given section ID number.

Table 129: *GET Preprocessing Items, Entity = ELEM

`Entity` = ELEM, `ENTNUM` = `N` (element number)
GET, `Par`, ELEM, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NODE	1, 2, ... 20	Node number at position 1,2,... or 20 of element`N`. Alternative get function: NELEM(`n,npos`), where `npos` is 1,2,...20.
CENT	X, Y, Z	Centroid X, Y, or Z location (based on shape function) in the active coordinate system. The original locations is used even if large deflections are active. Alternative get functions: CENTRX(`N`), CENTRY(`N`), and CENTRZ(`N`) always retrieve the element centroid in global Cartesian coordinates, and are determined from the selected nodes on the elements.
ADJ	1, 2, ... 6	Element number adjacent to face 1,2,...6. Alternative get function: ELADJ(`N`,`face`). Only elements (of the same dimensionality) adjacent to lateral faces are considered.
ATTR	`Name`	Number assigned to the attribute `Name`, where `Name` = MAT, TYPE, REAL, ESYS, PSTAT, LIVE, or SECN. Returns a zero if the element is unselected. If `Name` = LIVE, returns a 1 if the element is selected and active, and a -1 if it is selected and inactive. `Name` = SECN returns the section number of the selected beam element. `Name` = ISOLID returns the underlying element number of the selected contact or target element. A CNCHECK command is needed before the *GET command.
LENG		Length of line element (straight line between ends).
LPROJ	X, Y, Z	Projected line element length (in the active coordinate system). X is x-projection onto y-z plane, Y is y projection onto z-x plane, and Z is z-projection onto x-y plane.
AREA		Area of area element.
APROJ	X, Y, Z	Projected area of area element area (in the active coordinate system). X is x-projection onto y-z plane, Y is y projection onto z-x plane, and Z is z-projection onto x-y plane.
VOLU		Element volume. Based on unit thickness for 2D plane elements (unless the thickness option is used) and on the full 360 degrees for 2D axisymmetric elements. For general axisymmetric elements SOLID272 and SOLID273, only the area of the element on the master plane is reported before solving, not the volume. After solving, the volume is reported. Note: If results data are in the database, the volume returned is the volume calculated during solution.
ESEL		Select status of element `N`: -1 = unselected, 0 = undefined, 1 = selected. Alternative get function: ESEL(`N`).
NXTH		Next higher element number above `N` in selected set (or zero if none found). Alternative get function: ELNEXT(`N`)
NXTL		Next lower element number below `N` in selected set (or zero if none found).
HGEN		Heat generation on selected element `N`.
DGEN		Diffusing substance generation on selected node N (returns 0.0 if node is unselected, or if the DOF is inactive).
HCOE	face	Heat coefficient for selected element `N` on specified face. Returns the value at the first node that forms the face.
TBULK	face	Bulk temperature for selected element `N` on specified face. Returns the value at the first node that forms the face.
PRES	face	Pressure on selected element, `N` on specified face. Returns the value at the first node that forms the face.
SHPAR	`Test`	Element shape test result for selected element `N`, where `Test` = ANGD, ASPE (aspect ratio), JACR (Jacobian ratio), MAXA (maximum corner angle), PARA (deviation from parallelism of opposite edges), or WARP (warping factor).
MEMBER	COUNT	Number of reinforcing members (individual reinforcings) in the element `N`.
EGID	COUNT	Number of non-duplicate global identifiers in the element `N`.
EGID	MIN, MAX	Lowest or highest global identifier in the element `N`.

`Entity` = ELEM, `ENTNUM` = 0 (or blank)
GET, `Par`, ELEM, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX,MIN	Highest or lowest element number in the selected set.
NUM	MAXD, MIND	Highest or lowest element number defined.
COUNT		Number of elements in the selected set.
MATM		Highest material number that is referenced by an element.
TYPM		Highest element type number that is referenced by an element.
RELM		Highest real constant number that is referenced by an element.
ESYM		Highest element coordinate system number that is referenced by an element.
SECM		Highest section ID number that is referenced by an element.
PRTM		Highest part number that is referenced by an element.
MEMBER	COUNT	Number of reinforcing members (individual reinforcings) in the selected set of reinforcing elements.
EGID	COUNT	Number of non-duplicate global identifiers in the selected set of reinforcing elements.
	MIN, MAX	Lowest or highest global identifier in the selected set of reinforcing elements.
	MIND, MAXD	Lowest or highest global identifier defined.

Table 130: *GET Preprocessing Items, Entity = ETYP

`Entity` = ETYP, `ENTNUM` = `N` (element type number)
GET, `Par`, ETYP, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ATTR	`Name`	Number assigned to the attribute `Name`, where `Name`=ENAM, KOP1, KOP2, ..., KOP9, KO10, KO11, etc.

`Entity` = ETYP, `ENTNUM` = 0 (or blank)
GET,`Par`,ETYP, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX	Maximum element type.

Table 131: *GET Preprocessing Items, Entity = GCN

Entity = GCN, ENTNUM = 0 (or blank)

*GET, Par, GCN, 0, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

MAT Sect1 Item2 = 0 or blank; IT2NUM = Sect2. Material ID to be used for general contact between Sect1 and Sect2. Alternative get function: SECTOMAT(Sect1,Sect2).

REAL Sect1 Item2 = 0 or blank; IT2NUM = Sect2. Real constant ID to be used for general contact between Sect1 and Sect2. Alternative get function: SECTOREAL(Sect1,Sect2).

DEF

Sect1

Item2 = 0 or blank; IT2NUM = Sect2. Number indicating the type of contact for the general contact definition between Sect1 and Sect2:

= 0 - Excluded general contact between Sect1 / Sect2

= 1 - Asymmetric general contact between Sect1 (contact) / Sect2 (target)

= 2 - Asymmetric general contact between Sect1 (target) / Sect2 (contact)

= 3 - Symmetric general contact between Sect1 / Sect2

Sect1 and Sect2 are section numbers associated with general contact surfaces.

Table 132: *GET Preprocessing Items, Entity = GENB

Entity = GENB, ENTNUM =N (nonlinear beam general section identification number)

*GET, Par, GENB, N, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

COUNT (Blank) Number of defined sections. If Item1 = COUNT, then N is blank.

NUM MAX Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS (Blank) Returns a 1 if the section exists and if it is a GENB section.

SUBTYPE (Blank) Section subtype for the section ID specified via the SECTYPE command.

NAME (Blank) The 8-character section name defined via the SECTYPE command.

One of the following:

BSAX

BSM1

BSM2

BSTQ

BSS1

BSS2

BSMD

BSTE

(Blank)

Item2 = NTEM, the number of temperatures for BSAX, BSM1, BSM2, BSTQ, BSS1, BSS2, BSMD, or BSTE data.

One of the following:

BSAX

BSM1

BSM2

BSTQ

BSS1

BSS2

BSMD

BSTE

(Blank)

Item2 = TVAL; IT2NUM = nnn

Where nnn is the temperature value (<= NTEM).

One of the following:

BSAX

BSM1

BSM2

BSTQ

BSS1

BSS2

BSMD

BSTE

nnn

Item2 = TEMP; IT2NUM = tval

Where nnn is the location in the BSAX, BSM1, BSM2, BSTQ, BSS1, BSS2, BSMD, or BSTE command for the given coefficient number, and tval is the temperature value.

Examples for nnn:

nnn = 1 for STRAIN(1)

nnn = 2 for STRESS(1)

nnn = 3 for STRAIN(2)

nnn = 4 for STRESS(2)

nnn = 5 for STRAIN(3)

...

One of the following:

BSAX

BSM1

BSM2

BSTQ

BSS1

BSS2

BSMD

BSTE

(Blank)

Item2 = TEMP; IT2NUM = tval; Item3 = NCONST

The number of constants at tval.

Table 133: *GET Preprocessing Items, Entity = GENS

Entity = GENS, ENTNUM =N (preintegrated shell general section identification number)

*GET, Par, GENS, N, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

COUNT (Blank) Number of defined sections. If Item1 = COUNT, then N is blank.

NUM MAX Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS (Blank) Returns a 1 if the section exists and if it is a GENS section.

NAME (Blank) The 8-character section name defined via the SECTYPE command.

One of the following:

SSPA

SSPB

SSPD

SSPE

SSMT

SSBT

SSPM

(Blank)

Item2 = NTEM, the number of temperatures for SSPA, SSPB, SSPD, SSPE, SSMT, SSBT, or SSPM data.

One of the following:

SSPA

SSPB

SSPD

SSPE

SSMT

SSBT

SSPM

(Blank)

Item2 = TVAL; IT2NUM = nnn

Where nnn is the temperature value (<= NTEM).

One of the following:

SSPA

SSPB

SSPD

SSPE

SSMT

SSBT

SSPM

nnn

Item2 = TEMP; IT2NUM = tval

Where nnn is the location in the SSPA, SSPB, SSPD, SSPE, SSMT, SSBT, or SSPM command for the given coefficient number, and tval is the temperature value.

Table 134: *GET Preprocessing Items, Entity = KP

`Entity` = KP, `ENTNUM` = `N` (keypoint number)
GET, `Par`, KP, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
LOC	X, Y, Z	X, Y, or Z location in the active coordinate system. Alternative get functions: KX(`N`), KY(`N`), KZ(`N`). Inverse get function: KP(`x,y,z`) returns the number of the selected keypoint nearest the `x,y,z` location (in the active coordinate system, lowest number for coincident keypoints).
ATTR	`Name`	Number assigned to the attribute `Name`, where `Name` = MAT, TYPE, REAL, ESYS, NODE, or ELEM.
KSEL		Select status of keypoint `N`: -1 = unselected, 0 = undefined, 1 = selected. Alternative get function: KSEL(`N`).
NXTH		Next higher keypoint number above `N` in selected set (or zero if none found). Alternative get function: KPNEXT(`N`).
NXTL		Next lower keypoint number below `N` in selected set (or zero if none found).
DIV		Divisions (element size setting) from KESIZE command.

`Entity` = KP, `ENTNUM` = 0 (or blank)
GET, `Par`, KP, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX, MIN	Highest or lowest keypoint number in the selected set.
NUM	MAXD, MIND	Highest or lowest keypoint number defined
COUNT		Number of keypoints in the selected set.
CENT	X, Y, Z	Centroid X, Y, or Z location of keypoints (from last KSUM or GSUM).
IOR	X, Y, Z, XY, YZ, ZX	Moments of inertia about origin (from last KSUM or GSUM).
IMC	X, Y, Z, XY, YZ, ZX	Moments of inertia about mass centroid (from last KSUM or GSUM).
IPR	X, Y, Z	Principal moments of inertia (from last KSUM or GSUM).
IXV	X, Y, Z	Principal orientation X vector components (from last KSUM or GSUM).
IYV	X, Y, Z	Principal orientation Y vector components (from last KSUM or GSUM).
IZV	X, Y, Z	Principal orientation Z vector components (from last KSUM or GSUM).
MXLOC	X, Y, Z	Maximum X, Y, or Z keypoint coordinate in the selected set (in the active coordinate system).
MNLOC	X, Y, Z	Minimum X, Y, or Z keypoint coordinate in the selected set (in the active coordinate system).
NRELM	m	Keypoint number of meshed region nearest centroid of element `m`.

Table 135: *GET Preprocessing Items, Entity = LINE

`Entity` = LINE, `ENTNUM` = `N` (line number)
GET, `Par`, LINE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
KP	1,2	Keypoint number at position 1 or 2.
ATTR	`Name`	Number assigned to the attribute, `Name`, where `Name`=MAT, TYPE, REAL, ESYS, NNOD, NELM, NDIV, NDNX, SPAC, SPNX, KYND, KYSP, LAY1, or LAY2. (NNOD=number of nodes, returns --1 for meshed line with no internal nodes, NELM=number of elements, NDIV=number of divisions in an existing mesh, NDNX=number of divisions assigned for next mesh, SPAC=spacing ratio in an existing mesh, SPNX=spacing ratio for next mesh, KYND=soft key for NDNX, KYSP=soft key for SPNX, LAY1=LAYER1 setting, LAY2=LAYER2 setting.)
LSEL		Select status of line `N`: -1=unselected, 0=undefined, 1=selected. Alternative get function: LSEL(`N`).
NXTH		Next higher line number above `N` in the selected set (or zero if none found). Alternative get function: LSNEXT(`N`)
NXTL		Next lower line number below `N` in selected set (or zero if none found).
LENG		Length. A get function LX(`n,lfrac`) also exists to return the X coordinate location of line `N` at the length fraction `lfrac` (0.0 to 1.0). Similar LY and LZ functions exist.

`Entity` = LINE, `ENTNUM` = 0 (or blank)
GET, `Par`, LINE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX, MIN	Highest or lowest line number in the selected set.
NUM	MIND, MAXD	Highest or lowest line number defined.
COUNT		Number of lines in the selected set.
LENG		Combined length of lines (from last LSUM or GSUM).
CENT	X, Y, Z	Centroid X, Y, or Z location of lines (from last LSUM or GSUM).
IOR	X, Y, Z, XY, YZ, ZX	Moments of inertia about origin (from last LSUM or GSUM).
IMC	X, Y, Z, XY, YZ, ZX	Moments of inertia about mass centroid (from last LSUM or GSUM).
IPR	X, Y, Z	Principal moments of inertia (from last LSUM or GSUM).
IXV	X, Y, Z	Principal orientation X vector components (from last LSUM or GSUM).
IYV	X, Y, Z	Principal orientation Y vector components (from last LSUM or GSUM).
IZV	X, Y, Z	Principal orientation Z vector components (from last LSUM or GSUM).

Table 136: *GET Preprocessing Items, Entity = LINK

`Entity` = LINK, `ENTNUM` = 0 (or blank)
GET, `Par`, LINK, `NUM`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT		Number of defined sections.
NUM	MAX	Largest section number defined.

`Entity` = LINK, `ENTNUM` = `id` (link section identification number)
GET, `Par`, LINK, `id`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Section type (SECTYPE) (always LINK for link sections) associated with the section identified via `id`
NAME		Name defined for the given section identification number
DATA	`nnn`	Location in the SECDATA command for the given `id`
PROP	AREA	Area value
	ADDMAS	Added mass per unit length
	TENSKEY	Tension/compression key

Table 137: *GET Preprocessing Items, Entity = MAT

`Entity` = MAT, `ENTNUM` = 0 (or blank)
GET, `Par`, MAT, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT		Number of materials.
NUM	MAX	Largest material number for which at least one property is defined.

Table 138: *GET Preprocessing Items, Entity = MPLAB

`Entity` = MPlab, `ENTNUM` =`N` (`MPlab` = material property label from MP command; `N` = material number.)
GET, `Par`, MPlab, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TEMP	val	Material property value at temperature of `val`. For temperature dependent materials, the program interpolates the property at temperature input for `val`.

Table 139: *GET Preprocessing Items, Entity = NODE

`Entity` = NODE, `ENTNUM` = `N` (node number)
GET, `Par`, NODE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
LOC	X, Y, Z	X, Y, Z location in the active coordinate system. Alternative get functions: NX(`N`), NY(`N`), NZ(`N`). Inverse get function. NODE(`x,y,z`) returns the number of the selected node nearest the `x,y,z` location (in the active coordinate system, lowest number for coincident nodes).
ANG	XY, YZ, ZX	THXY, THYZ, THZX rotation angle.
NSEL		Select status of node `N`: -1=unselected, 0=undefined, 1=selected. Alternative get function: NSEL(`N`).
NXTH		Next higher node number above `N` in selected set (or zero if none found). Alternative get function: NDNEXT(`N`).
NXTL		Next lower node number below `N` in selected set (or zero if none found).
F	FX, MX, ...	Applied force at selected node `N` in direction `IT1NUM` (returns 0.0 if no force is defined, if node is unselected, or if the DOF is inactive). If `ITEM2` is IMAG, return the imaginary part. If the applied force is defined as a constant for this load step, regardless of the KBC setting, the result will be the force at the end time of a load step.
D	UX, ROTX, ...	Applied constraint force at selected node `N` in direction `IT1NUM` (returns a large number, such as 2e100, if no constraint is specified, if the node is unselected, or if the DOF is inactive). If `ITEM2` is IMAG, return the imaginary part. If the applied constraint force is defined as a constant for this load step, regardless of the KBC setting, the result will be the force at the end time of a load step.
HGEN		Heat generation on selected node `N` (returns 0.0 if node is unselected, or if the DOF is inactive).
NTEMP		Temperature on selected node N (returns 0.0 if node is unselected)
CPS	Lab	Couple set number with direction Lab = any active DOF, which contains the node `N`.
DGEN		Diffusing substance generation on selected node N (returns 0.0 if node is unselected, or if the DOF is inactive).

`Entity` = NODE, `ENTNUM` = 0 (or blank)
GET, `Par`, NODE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NUM	MAX, MIN	Highest or lowest node number in the selected set.
NUM	MAXD, MIND	Highest or lowest node number defined.
COUNT		Number of nodes in the selected set.
MXLOC	X, Y, Z	Maximum X, Y, or Z node coordinate in the selected set (in the active coordinate system).
MNLOC	X, Y, Z	Minimum X, Y, or Z node coordinate in the selected set (in the active coordinate system).
Note: If the application creates internal nodes during solution, the internal nodes will not be included. You can include them by using `KINTERNAL`. The command syntax is: GET, `Par`, NODE, 0, Item1, IT1NUM, Item2, IT2NUM, KINTERNAL The options for the `KINTERNAL`* key are (blank), which counts all nodes except internal nodes, and INTERNAL, which counts all nodes including internal nodes.

Table 140: *GET Preprocessing Items, Entity = OCEAN

`Entity` = OCEAN, `ENTNUM` = `Type` (where `Type` is a valid label on the `DataType` field of the OCTYPE command)
GET, `Par`, OCEAN, `Type`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NAME		Name defined for a given `Type`
DATA	1	Depth when `Type` = BASI
	2	Material ID when `Type` = BASI
	8	`KFLOOD` when `Type` = BASI
	9	`Cay` when `Type` = BASI
	10	`Cb` when `Type` = BASI
	11	`Zmsl` when `Type` = BASI
	13	`Caz` when `Type` = BASI
	14	`Ktable` when `Type` = BASI
	1	`KWAVE` when `Type` = WAVE
	2	`THETA` when `Type` = WAVE
	3	`WAVELOC` when `Type` = WAVE
	4	`KCRC` when `Type` = WAVE
	5	`KMF` when `Type` = WAVE
	6	`PRKEY` when `Type` = WAVE
PROP	NROW	Number of rows defined by OCTABLE command
TABL	`i`	Data in table defined by OCTABLE command `i` = row number; Item2 = column number

`Entity` = OCEAN, `ENTNUM` = 0 (or blank)
GET, `Par`, OCEAN, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
COUNT		Number of defined global ocean entities (BASIC/CURRENT/WAVE)
It may be necessary to determine `Cay`, `Caz`, `CMy`, or `CMz` during the solution process. In such cases, a negative value (-1.0) is returned to `Par` if the item is not specified in the database.

Table 141: *GET Preprocessing Items, Entity = OCZONE

`Entity` = OCZONE, `ENTNUM` = `Name` (where `Name` is a valid label on the `ZoneName` field of the OCZONE command)
GET, `Par`, OCZONE, `Name`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
DATA	8	`KFLOOD` for a given `ENTNUM` = `Name`
	9	`Cay` for a given `ENTNUM` = `Name`
	10	`Cb` for a given `ENTNUM` = `Name`
	13	`Caz` for a given `ENTNUM` = `Name`
PROP	NROW	Number of rows defined by OCTABLE command
TABL	`i`	Data in table defined by OCTABLE command `i` = row number; Item2 = column number
TYPE		Ocean zone type (returns 1, 2 or 3 for ZLOC-, COMP-, or PIP-type zones, respectively)
COMP		Component name when the given ocean zone type is COMP, or internal component name when the given ocean zone type is PIP
COMP2		External component name when the type of given ocean zone is PIP

`Entity` = OCZONE, `ENTNUM` = `N`
GET, `Par`, OCZONE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
NAME		Name defined for a given zone ID (`ENTNUM`)

`Entity` = OCZONE, `ENTNUM` = 0 (or blank)
GET, `Par`, OCZONE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
COUNT		Number of defined zones
If a requested item is not specified in the database, a negative value (-1.0) is returned to `Par`.

Table 142: *GET Preprocessing Items, Entity = PIPE

`Entity` = PIPE, `ENTNUM` = 0 (or blank)
GET, `Par`, PIPE, `NUM`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT		Number of defined sections
NUM	MAX	Largest section number defined

`Entity` = PIPE, `ENTNUM` = `id` (pipe section identification number)
GET, `Par`, PIPE, `id`*, Item1, IT1NUM, Item2, IT2NUM
Item1	IT1NUM	Description
TYPE		Section type, for id - SECTYPE command (always PIPE for pipe sections)
SUBTYPE		Section type for id - SECTYPE command
NAME		Name defined for the given section id number
DATA	`nnn`	Where `nnn` is the location in the SECDATA command for the given section id number
SFLEX	`nnn`	Where `nnn` is the location in the SFLEX command for the given section ID number
PROP	AREA	Area value
	IYY, IYZ, IZZ	Moments of inertia
	TORS	Torsion constant
	SCYY, SCYZ, SCZZ	Shear correction factors
	OFFY	Section offset in the Y direction.
	OFFZ	Section offset in the Z direction.
	ADDMAS	Added mass per unit length

Table 143: *GET Preprocessing Items, Entity = PART

`Entity` = PART, `ENTNUM` = `N` (PART number)
GET, `Par`, PART, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Element type number assigned to PART `N`.
MAT		Material number assigned to PART `N`.
REAL		Real constant number assigned to PART `N`.

`Entity` = PART, `ENTNUM` = 0 (or blank)
GET, `Par`*, PART, 0, Item1, IT1NUM, Item2, IT2NUM
NUMP		Total number of parts in the model.

Table 144: *GET Preprocessing Items, Entity = RCON

`Entity` = RCON, `ENTNUM` = `N` (real constant set number)
GET, `Par`, RCON, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
CONST	1, 2, ..., `m`	Value of real constant number `m` in set `N`.
GET, `Par`, RCON, `0`*, Item1, IT1NUM, Item2, IT2NUM
NUM	MAX	The maximum real constant set number defined

Table 145: *GET Preprocessing Items, Entity = REIN

`Entity` = REIN, `ENTNUM` = `N` (reinforcing section identification number)
GET, `Par`, REIN, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Section type, for ID -- SECTYPE command (always REIN for reinforcing sections).
SUBTYPE		Section subtype for ID -- SECTYPE command.
NAME		Name defined for a given ID number.
NREIN		Number of reinforcing fibers. For reinforcing sections generated (EREINF) via the standard method, the number of fibers defined via SECDATA. For reinforcing sections generated (EREINF) via the mesh-independent method, the total number of fibers in the section.
TABL	`ReinfNum,I`	Reinforcing fiber data, as defined via SECDATA. This item is not allowed for reinforcing sections generated (EREINF) via the mesh-independent method.

Table 146: *GET Preprocessing Items, Entity = SCTN

`Entity` = SCTN, `ENTNUM` = `N` (pretension section ID number)
GET, `Par`, SCTN, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
1		Section ID number.
2		Section type (always 5 for pretension section).
3		Pretension node number.
4	Coordinate system number.	Section normal NX.
5	Coordinate system number.	Section normal NY.
6	Coordinate system number.	Section normal NZ.
7 or 8		Eight character section name.
9		Initial action key. Returns 0 or 1 for lock, 2 for "free-to-slide," or 3 for tiny.
10		Force displacement key. Returns 0 or 1 for force, or 2 for displacement.
11		First preload value.
12		Load step in which first preload value is to be applied.
13		Load step in which first preload value is to be locked.
14...		14 through 17 is a repeat of 10 through 13, but for the second preload value; 18 through 21 is for the third preload value; and so forth.

Table 147: *GET Preprocessing Items, Entity = SECP

`Entity` = SECP, `ENTNUM` = 0 (or blank)
GET, `Par`, SECP, `NUM`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
COUNT		Number of defined sections
NUM	MAX	Largest section number defined

Entity = SECP, ENTNUM = id (beam section identification number)

*GET, Par, SECP, id, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

TYPE Section type, for id - SECTYPE command (always BEAM for beam sections)

SUBTYPE Section type for id - SECTYPE command

NAME Name defined for the given section id number

DATA nnn Where nnn is the location in the SECDATA command for the given section id number

PROP AREA Area value

IYY, IYZ, IZZ Moments of inertia

WARP Warping constant

TORS Torsion constant

CGY, CGZ Y or Z coordinate center of gravity

SHCY, SHCZ Y or Z coordinate shear center

SCYY, SCYZ, SCZZ Shear correction factors

OFFSET

Offset location:

1 = Centroid

2 = Shear Center

3 = Origin

0 = User Defined

OFFY Section offset in the Y direction.

OFFZ Section offset in the Z direction.

TXY User transverse shear stiffness XY

TXZ User transverse shear stiffness XZ

ADDMAS Added mass per unit length

Table 148: *GET Preprocessing Items, Entity = SHEL

`Entity` = SHEL, ENTNUM = `N` (shell section identification number)
GET, `Par`, SHEL, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
TYPE		Section type, for id -- SECTYPE command. (always SHEL for shell sections)
NAME		Name defined for a given id number.
PROP	TTHK	Total thickness.
	NLAY	Number of layers.
	NSP	Number of section integration points.
	POS	Node position (as defined by SECOFFSET).
		0 = User Defined.
		1 = Middle.
		2 = Top.
		3 = Bottom.
	OFFZ	User-defined section offset (POS = 0).
	TS11	Transverse shear stiffness factors.
	TS22	Transverse shear stiffness factors.
	TS12	Transverse shear stiffness factors.
	HORC	Homogeneous or complete section flag.
		0 = Homogeneous.
		1 = Composite.
	FUNC	Tabular function name for total thickness.
	UT11	User transverse shear stiffness 11.
	UT22	User transverse shear stiffness 22.
	UT12	User transverse shear stiffness 12.
	AMAS	Added mass.
	MSCF	Hourglass control membrane scale factor.
	BSCF	Hourglass control bending scale factor.
	DSTF	Drill stiffness scale factor.
	LDEN	Laminate density.
	FKCN	`KCN` field value from the SECFUNCTION command, in which the array or table is interpreted.
	ABD	Section membrane and bending stiffness matrix. Valid ITEM2 = 1,6 and IT2NUM = 1,6.
	E	Section transverse shear stiffness matrix. Valid ITEM2 = 1,2 and IT2NUM = 1,2.
LAYD	LayerNumber,THIC	Layer thickness.
	LayerNumber,MAT	Layer material.
	LayerNumber,ANGL	Layer orientation angle.
	LayerNumber,NINT	Number of layer integration points.

Table 149: *GET Preprocessing Items, Entity = TBFT

`Entity` = TBFT, `ENTNUM` = `blank`
GET, `Par`, TBFT, , `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
nmat		Number of defined material models.
matnum	`index`	Material number in array (index varies for 1 to num materials).
`Entity` = TBFT, `ENTNUM` = `matid` (For getting names of constitutive function, matid = the material ID number)
GET, `Par`, TBFT, `matid`, `nfun`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
nfun		Number of constitutive functions for this material.
`Entity` = TBFT, `ENTNUM` = `matid` (To query constitutive function data, matid = the material ID number)
GET, `Par`, TBFT, `matid`, `func`, `fname`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
func	index	If Item2 = fname, the name of the constitutive function is returned.
func	function name	If Item2 = ncon, the number of constants is returned for the function specified in IT1NUM by the constitutive function name.
"	"	If Item2 = cons, set Item2num to index to return the value of the constant.
"	"	If Item2 = fixe, set Item2num to index to return the fix flag status.
"	"	If Item2 = RESI, returns the residual error while fitting the data.
"	"	If Item2 = type, returns the category of the constitutive model (moon, poly, etc.)
"	"	If Item2 = sord, returns the shear order of the prony visco model.
"	"	If Item2 = bord, returns the bulk order of the prony visco model.
"	"	If Item2 = shif, returns the shift function name of the prony visco model.
`Entity` = TBFT, `ENTNUM` = `matid` (For getting names of experimental data, matid = the material ID number)
GET, `Par`, TBFT, `matid`, `nexp`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
nexp		Number of experiments for this material.
`Entity` = TBFT, `ENTNUM` = `matid` (To query experimental data, `matid` = the material ID number))
GET, `Par`, TBFT, `matid`, `func`, `fname`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
"	expindex	If Item2 = type, returns experiments type string.
"	"	If Item2 = numrow, returns number of rows in the data.
"	"	If Item2 = numcol, returns the number of cols in a row (set Intem2num = Row index)
"	"	If Item2 = data, returns the value of the data in row, col of exp expindex (set item2Num = row index and item3 = column index. All indices vary from 1 to the maximum value.
"	"	If Item2 = natt, returns the number of attributes.
"	"	If Item2 = attname, returns the attribute name (set Item2Num = Attr index).
"	"	If Item2 = attvald, returns double value of attribute (set Item2Num = Attr index).
"	"	If Item2 = attvali, returns integer valud of attribute (set Item2Num = Attr index).
"	"	If Item2 = attvals, returns the string value of the attribute (set Item2Num = Attr index).

Table 150: *GET Preprocessing Items, Entity = TBLAB

`Entity` = TBLAB, `ENTNUM` = `N`..(`TBlab` = data table label from the TB command; `N` = material number.)
GET, `Par`, `TBlab`, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`, `TBOPT`*
Item1	IT1NUM	Description
TEMP	`T`	Item2: CONST IT2NUM: `Num` Value of constant number Num in the data table at temperature `T`. For constants, input an X,Y point; the constant numbers are consecutive with the X constants being the odd numbers, beginning with one.
Important: To get all necessary output for materials defined via the TB command, you must specify the final argument `TBOPT` as indicated in the syntax description above.

Table 151: *GET Preprocessing Items, Entity = VOLU

`Entity` = VOLU, `ENTNUM` = `N` (volume number)
GET, `Par`, VOLU, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ATTR	`Name`	Number assigned to the attribute `Name`, where `Name`=MAT, TYPE, REAL, ESYS, NNOD, or NELM. (NNOD=number of nodes, NELM=number of elements.)
VSEL		Select status of volume `N`: -1=unselected, 0=undefined, 1=selected. Alternative get function: VSEL(`N`).
NXTH		Next higher volume number above `N` in selected set (or zero if none found). Alternative get function: VLNEXT(`N`).
NXTL		Next lower volume number below `N` in selected set (or zero if none found).
VOLU		Volume of volume `N`. (VSUM or GSUM must have been performed sometime previously with at least this volume `N` selected).
SHELL	1, 2, ..., `m`	Item2: AREA IT2NUM: 1,2,...,`p` Line number of position `p` of shell `m`

`Entity` = VOLU, `ENTNUM` = 0 (or blank)
GET, `Par`*, VOLU, 0, Item1, IT1NUM, Item2, IT2NUM
NUM	MAX, MIN	Highest or lowest volume number in the selected set.
NUM	MAXD, MIND	Highest or lowest volume number defined.
COUNT		Number of volumes in the selected set.
VOLU		Combined volumes (from last VSUM or GSUM).
CENT	X, Y, Z	Centroid X, Y, or Z location of volumes (from last VSUM or GSUM).
IOR	X, Y, Z, XY, YZ, ZX	Moments of inertia about origin (from last VSUM or GSUM).
IMC	X, Y, Z, XY, YZ, ZX	Moments of inertia about mass centroid (from last VSUM or GSUM).
IPR	X, Y, Z	Principal moments of inertia (from last VSUM or GSUM).
IXV	X, Y, Z	Principal orientation X vector components (from last VSUM or GSUM).
IYV	X, Y, Z	Principal orientation Y vector components (from last VSUM or GSUM).
IZV	X, Y, Z	Principal orientation Z vector components (from last VSUM or GSUM).

Solution Items

*GET Solution Entity Items

Table 152: *GET Solution Items, Entity = ACTIVE

`Entity` = ACTIVE, `ENTNUM` = 0 (or blank)
GET, `Par`, ACTIVE, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ANTY		Current analysis type.
SOLU	DTIME	Time step size.
	NCMLS	Cumulative number of load steps.
	NCMSS	Number of substeps. NOTE: Used only for static, transient, and harmonic balance method (HBM) analyses.
	EQIT	Number of equilibrium iterations.
	NCMIT	Cumulative number of iterations.
	CNVG	Convergence indicator: 0=not converged, 1=converged.
	MXDVL	Maximum degree of freedom value.
	RESFRQ	Response frequency for 2nd order systems.
	RESEIG	Response eigenvalue for 1st order systems.
	DSPRM	Descent parameter.
	FOCV	Force convergence value.
	MOCV	Moment convergence value.
	HFCV	Heat flow convergence value.
	MFCV	Magnetic flux convergence value.
	CSCV	Current segment convergence value.
	CUCV	Current convergence value.
	FFCV	Fluid flow convergence value.
	DICV	Displacement convergence value.
	ROCV	Rotation convergence value.
	TECV	Temperature convergence value.
	VMCV	Vector magnetic potential convergence value.
	SMCV	Scalar magnetic potential convergence value.
	VOCV	Voltage convergence value.
	PRCV	Pressure convergence value.
	VECV	Velocity convergence value.
	CRPRAT	Maximum creep ratio.
	PSINC	Maximum plastic strain increment.
	CGITER	Number of iterations in the PCG and symmetric JCG (non-complex version) solvers.

Table 153: *GET Solution Items, Entity = ELEM

`Entity` = ELEM, `ENTNUM` = 0 (or blank)
GET, `Par`, ELEM, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
MTOT	X, Y, Z	Total mass components.
MC	X, Y, Z	Center of mass components.
IOR	X, Y, Z, XY, YZ, ZX	Moment of inertia about origin.
IMC	X, Y, Z, XY, YZ, ZX	Moment of inertia about the center of mass.
IPRIN	X, Y, Z	Principal moments of inertia.
IANG	XY, YZ, ZX	Angles of the moments of inertia principal axes.
FMC	X, Y, Z	Force components at mass centroid (1).
MMOR	X, Y, Z	Moment components at origin (1).
MMMC	X, Y, Z	Moment components at mass centroid (1).

Note: Items (1) are available only after inertia relief solution (IRLF,1) or pre-calculation of masses (IRLF,-1).

Item values are consistent with the mass summary printed in the output file. They are based on unscaled mass properties (see MASCALE command).

Table 154: *GET Solution Items, Entity = MODE

`Entity` = MODE, `ENTNUM` = `N` (mode number)
GET, `Par`, MODE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
FREQ		Frequency of mode `N`. Returned values are valid for modal analyses which calculate real eigensolutions.
STAB		Stability value of mode `N`. Returned values are valid for modal analyses which calculate complex eigensolutions. The stability value is the real part of the complex eigenvalue. It contains information on the mode damping in a damped modal analysis.
DFRQ		Damped frequency of mode `N`. Returned values are valid for modal analyses which calculate complex eigensolutions. The damped frequency is the imaginary part of the complex eigenvalue.
PFACT		Participation factor of mode `N`. If retrieved after a modal analysis, the real part of the participation factor is returned unless `IT1NUM` = IMAG. The direction is specified using `Item2` = DIREC and `IT2NUM` = X, Y, Z, ROTX, ROTY, or ROTZ If retrieved after a spectrum analysis, the spectrum number M is specified using `Item2` = SPECT and `IT2NUM` = M. For a PSD analysis with spatial correlation or wave excitation, the retrieved participation factors will correspond to the first degree of freedom that is excited.
EFFM		Effective mass of mode `N`. Returned values are valid only after a modal analysis with effective mass calculation has been solved. The direction is specified using `Item2` = DIREC and `IT2NUM` = X, Y, Z, ROTX, ROTY, or ROTZ.
GENM		Generalized mass (also called modal mass) of mode `N`. Returned values are valid only after a modal analysis with generalized mass calculation has been solved.
MCOEF		Mode coefficient of mode `N`. Returned values are valid only after a spectrum analysis has been solved. The spectrum number M is specified using `Item2` = SPECT and `IT2NUM` = M. In a SPRS analysis, the values returned are based on the curve with the lowest damping. After a PSD analysis, the diagonal of the dynamic modal covariance matrix is retrieved for the displacement solution.
DAMP		Damping ratio of mode `N`. If retrieved after a modal analysis that creates complex solutions (DAMP, QRDAMP, or UNSYM eigensolvers) returned value is calculated from the complex frequencies. If retrieved after a spectrum analysis, returned value is the effective damping ratio. Not a function of direction. Also retrievable following a harmonic analysis or transient analysis with mode-superposition.

For all items except PFACT and MCOEF (as noted above), only the first 10000 values corresponding to significant modes will be returned.

The MODE file must be available to retrieve items PFACT and MCOEF with specified Item2. If Item2 is not specified, the last calculated value will be returned.

All values retrieved correspond to the first load step values. For a Campbell diagram analysis (multistep modal), *GET with Entity = CAMP must be used.

Table 155: *GET Solution Items, Entity = DDAM

`Entity` = DDAM, `ENTNUM` = `N` (mode number)
GET,`Par`,DDAM,`N`, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
DSHOCK		Shock design value of mode `N`.

If multiple DDAM analyses are performed, the last calculated value will be returned.

Postprocessing Items

*GET Postprocessing Entity Items

Table 156: *GET Postprocessing Items, Entity = ACTIVE

Entity = ACTIVE, ENTNUM = 0 (or blank)

*GET,Par, ACTIVE, 0, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

SET LSTP Current load step number.

SBST Current substep number.

TIME Time associated with current results in the database.

FREQ Frequency (for ANTYPE=MODAL, HARMIC, SPECTR; load factor for ANTYPE=BUCKLE).

NSET

If Item2 is blank, number of data sets on result file.

If Item2 = FIRST, IT2NUM = Loadstep, get set number of first substep of loadstep

If Item2 = LAST, IT2NUM = Loadstep, get set number of last substep of loadstep

RSYS Active results coordinate system.

Table 157: *GET Postprocessing Items, Entity = ACUS

`Entity` = ACUS, `ENTNUM` = 0 (or blank)
GET, `Par`, ACUS, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
PWL		Radiated sound power level
PRES		Far-field pressure at a given point
PHASE		Far-field pressure phase at a given point
SPL		Far-field sound pressure level at a given point
SPLA		Far-field a-weighted sound pressure level at a given point
DG		Far-field directivity at a given point
PS		Far-field scattered pressure at a given point
TS		Far-field target strength at a given point
DFIN		Diffuse sound field incident power
SIMP		Magnitude of specific acoustic impedance on the selected surface
AIMP		Magnitude of acoustic impedance on the selected surface
MIMP		Magnitude of mechanical impedance on the selected surface
APRES		Magnitude of average pressure on the selected surface
FORC		Magnitude of average force on the selected surface
POWER		Acoustic power through the selected surface
BSPL		SPL over frequency band
BSPA		A-weighted SPL over frequency band
PWRF		Reference sound power
TL		Transmission loss
RL		Return loss
Item1 = PWL, PRES, SPL, SPLA, PHASE, DG, PS, and TS are available after issuing the PRFAR or PLFAR command. The maximum values are obtained from the current command. Item1 = SIMP, AIMP, MIMP, APRES, FORC, POWER, TL, and RL are available after issuing the corresponding PRAS command at the current frequency. The values are obtained at the current frequency, or at the last frequency for multiple load step and substep cases. Item1 = DFIN is available after the diffuse sound field solution.

Table 158: *GET Postprocessing Items, Entity = CAMP

Note: Available after PLCAMP or PRCAMP command is issued. `Entity` = CAMP, `ENTNUM` = `N` (mode number)
GET,`Par`, CAMP, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NBMO		Number of modes in the Campbell diagram (`ENTNUM` not required). This value is the maximum value for `N`.
NBST		Number of steps in the Campbell diagram: modal load steps with rotational velocity (`ENTNUM` not required). This value is the maximum value for `M` (see Item1 = FREQ).
WHRL	`M`	Whirl of mode `N` at step `M`: -1 is backward whirl, 1 is forward whirl, and 0 is undetermined. For default `IT1NUM`, it corresponds to the whirl at the maximum rotational velocity.
VCRI		Critical speed for mode `N`. This value is available if an excitation is defined via the PLCAMP or PRCAMP command's `SLOPE` argument. (The unit of speed depends upon the `UNIT` value specified in those commands.) Note: N does not correspond to the mode number if `FREQB` (PRCAMP or PLCAMP command) is used. Instead, it represents the Nth mode number listed in the output of PRCAMP or PLCAMP.
FREQ	`M`	Natural frequency of mode (Hz) `N` at step `M`. It represents the complex part of the eigenvalue.
STAB	`M`	Stability value (Hz) of mode `N` at step `M`. It represents the real part of the eigenvalue.
UKEY	`M`	Instability key for mode `N` at step `M`: 0 is stable and 1 is unstable. For default `IT1NUM`, it corresponds to the stability over the whole rotational velocity range.
VSTA		Stability limit for mode N. This value is available when `SLOPE` is zero on the PLCAMP or PRCAMP command. (The unit of speed depends upon the `UNIT` value specified in those commands.) Note: N does not correspond to the mode number if `FREQB` (PRCAMP or PLCAMP command) is used. Instead, it represents the Nth mode number listed in the output of PRCAMP or PLCAMP.

Note: If the sorting is activated (Option=ON on the PRCAMP and PLCAMP commands), all the parameters retrieved are in the sorted order.

Table 159: *GET Postprocessing Items, Entity = CINT

`Entity` = CINT, `ENTNUM` = `CrackId` (required Crack ID number)
GET,`Par`, CINT, `CrackId`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
CTIP	ctnum	`IT1NUM` = Crack tip node number (required) `Item2` = CONTOUR `IT2NUM` = Contour number (default 1) Returns JINT value if crack ID is JINT type; otherwise, returns 0. `Item1` defaults to CTIP, `Item2` defaults to CONTOUR.
`Entity` = CINT, `ENTNUM` = CrackID (required Crack ID number)
GET, `Par`, CINT, `CrackId`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`, `Item3`, `IT3NUM`, `Item4`, `IT4NUM`*
Item1	IT1NUM	Description
CTIP	ctnum	`IT1NUM` = Crack tip node number (required) `Item2` = CONTOUR `IT2NUM` = Contour number (default 1) `Item3` = DTYPE `IT3NUM` = Data type (JINT, IIN1, IIN2, IIN3, K1, K2, K3, G1, G2, G3, GT, MFTX, MFTY, MFTZ, TSTRESS, CEXT, STTMAX, PSMAX, CSTAR, DLTA, DLTN, DLTK, KEQV, KANG, R, UFAC, CRDX, CRDY, CRDZ, and APOS) FOR `IT3NUM` = STTMAX or PSMAX: Item4 = AINDEX (angle index) IT4NUM = Index value (1 to N+1; N = Maximum number of intervals for the sweep (CINT,RSWEEP). Returns specified data type value. FOR `IT3NUM` = DLTA, DLTN, DLTK, KEQV, KANG, R, UFAC, CRDX, CRDY, CRDZ, APOS: Set `IT2NUM` = 1 Returns specified data type value. `Item1` defaults to CTIP, `Item2` defaults to CONTOUR, `Item3` defaults to DTYPE. Note: DLTK in a 3D XFEM-based fatigue crack-growth analysis is evaluated based on the smoothed SIFS values. The actual DLTK value can be easily calculated by issuing *GET for SIFS values and the stress (load) ratio.
`Entity` = CINT, `ENTNUM` = CrackID (required Crack ID number)
GET, `Par`, CINT, `CrackId`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*,
Item1	IT1NUM	Description
NNOD		Maximum number of nodes along the crack front.
`Entity` = CINT, `ENTNUM` = CrackID (required Crack ID number)
**GET, `Par`, CINT, `CrackId`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`***
Item1	IT1NUM	Description
NODE	ipos	IT1NUM = Position along the crack front (from 1 to NNOD). Default = 1. Returns node number at the given position along the crack front. (For XFEM, an internal node number is returned.)

Table 160: *GET Postprocessing Items, Entity = CYCCALC

`Entity` = CYCCALC, `ENTNUM` = CYCSPEC specification number Generate date for cyclic results using CYCCALC before retrieving those items.
GET,`Par`,CYCCALC,`spec`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Item2	IT2NUM	Description
FREQ	frequency point	SECTOR	sector	CYCSPEC result at the IT1NUM frequency and IT2NUM sector
		SECMAX	-	CYCSPEC maximum result at the IT1NUM frequency
		SECNUM	-	CYCSPEC sector with the maximum result at the IT1NUM frequency
		SECNODE	-	CYCSPEC node in the sector with the maximum result at the IT1NUM frequency
The frequency point refers to the harmonic solution data set number (NSET on the SET command)

Table 161: *GET Postprocessing Items, Entity = ELEM

`Entity` = ELEM, `ENTNUM` = `N` (element number)
GET,`Par`, ELEM, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
SERR^[a]		Structural error energy.
SDSG^[a]		Absolute value of the maximum variation of any nodal stress component.
TERR^[a]		Thermal error energy.
TDSG^[a]		Absolute value of the maximum variation of any nodal thermal gradient component.
SENE		"Stiffness" energy or thermal heat dissipation. Same as TENE.
TENE		Thermal heat dissipation or "stiffness" energy. Same as SENE.
KENE		Kinetic energy.
ASENE		Amplitude “stiffness” energy.
PSENE		Peak “stiffness” energy.
AKENE		Amplitude kinetic energy.
PKENE		Peak kinetic energy.
DENE		Damping energy.
WEXT^[b]		Work due to external load.
JHEAT		Element Joule heat generation (coupled-field calculation).
JS	X, Y, Z	Source current density (coupled-field calculation) in the global Cartesian coordinate system.
HS	X, Y, Z	Average element magnetic field intensity from current sources.
VOLU		Element volume, as calculated during solution.
ETAB	`Lab`	Value of element table item `Lab` for element `N` (see ETABLE command).
EFOR	`Nnum`	Element force at node `Nnum`. The force label is specified using Item2 = FX, FY, FZ, MX, MY, MZ, or HEAT. In a dynamics analysis, the element forces returned are based on the type of force requested. It is specified using the FORCE command for all dynamics analyses, except for spectrum analyses where `ForceType` is used on the combination commands (SRSS, PSDCOM, etc.).
SMISC	`Snum`	Value of element summable miscellaneous data at sequence number `Snum` (as used on ETABLE command).
NMISC	`Snum`	Value of element non-summable miscellaneous data at sequence number `Snum` (as used on ETABLE command).
FSOU		Element fluid flow source loading (poromechanics).

^[a]Some element- and material-type limitations apply. For more information, see the documentation for the PRERR command.

^[b]WEXT is calculated for element-based loading only (and not for nodal-force loading). WEXT is stored on elements to which loading has been applied; if surface elements are added on top of other elements, for example, and pressure loading is applied to the surface elements, WEXT is available for the surface elements only.

Table 162: *GET Postprocessing Items, Entity = ETAB

`Entity` = ETAB, `ENTNUM = N` (column number)
GET,`Par`, ETAB, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
LAB		Label for column `N` of the element table (ETABLE). Returns a character parameter.
ELEM	`E`	Value in ETABLE column `N` for element number `E`.

`Entity` = ETAB, `ENTNUM` = 0 (or blank)
GET,`Par`*,ETAB,0, Item1, IT1NUM, Item2, IT2NUM
Item1	IT1NUM	Description
NCOL	MAX	Total number of ETABLE columns.
NLENG	MAX	Largest element number defined.

Table 163: *GET Postprocessing Items, Entity = FSUM

`Entity` = FSUM, `ENTNUM` = 0 (or blank)
GET, `Par`, FSUM, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ITEM	`Lab`	Value of item `Lab` from last FSUM command. Valid labels are FX, FY, FZ, MX, MY, MZ, FLOW, HEAT, FLUX, etc.

Table 164: *GET Postprocessing Items, Entity = GSRESULT

`Entity` = GSRESULT, `ENTNUM` = 0 (or blank) for generalized plane strain results in fiber direction
GET, `Par`, GSRESULT, 0, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
LFIBER		Fiber length change at ending point.
ROT	X,Y	Rotation angle of end plane about X or Y axis.
F		Reaction force at ending point.
M	X,Y	Reaction moment on ending plane.

Table 165: *GET Postprocessing Items, Entity = MEMBER

`Entity` = MEMBER, `ENTNUM` = `N` (GroupID)
GET,`Par`,MEMBER,`N`, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
TEMP	MIN, MAX	Minimum or maximum temperature of members (individual reinforcings) with GroupID = `N` in the selected set of reinforcing elements.

`Entity` = MEMBER, `ENTNUM` = 0 (or blank)
GET,`Par`,MEMBER,0, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
TEMP	MIN, MAX	Minimum or maximum temperature in the selected set of reinforcing elements.

Table 166: *GET Postprocessing Items, Entity = NODE

Entity = NODE, ENTNUM = N (node number) for nodal degree-of-freedom results:

*GET, Par, NODE, N, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Description

U X, Y, Z, SUM X, Y, or Z structural displacement or vector sum. Alternative get functions: UX(N), UY(N), UZ(N).

ROT X, Y, Z, SUM X, Y, or Z structural rotation or vector sum. Alternative get functions: ROTX(N), ROTY(N), ROTZ(N).

TEMP

Temperature. For SHELL131 and SHELL132 elements with KEYOPT(3) = 0 or 1, use TBOT, TE2, TE3, . . ., TTOP instead of TEMP. Alternative get functions: TEMP(N), TBOT(N), TE2(N), etc.

For SHELL294 element, use TBOT and TTOP in addition to TEMP. Alternative get functions: TEMP(N), TBOT(N), and TTOP(N).

PRES Pressure. Alternative get function: PRES(N).

GFV1, GFV2, GFV3 Nonlocal field values 1, 2, and 3.

VOLT Electric potential. Alternative get function: VOLT(N).

CONC Concentration.

MAG Magnetic scalar potential. Alternative get function: MAG(N).

V X, Y, Z, SUM X, Y, or Z fluid velocity or vector sum in a fluid analysis. X, Y, or Z nodal velocity or vector sum in a structural transient analysis (analysis with ANTYPE,TRANS). Alternative get functions: VX(N), VY(N), VZ(N).

A X, Y, Z, SUM X, Y, or Z magnetic vector potential or vector sum in an electromagnetic analysis. X, Y, or Z nodal acceleration or vector sum in a structural transient analysis (analysis with ANTYPE,TRANS). Alternative get functions: AX(N), AY(N), AZ(N).

CURR Current.

EMF Electromotive force drop.

RF FX, FY, FZ, MX, MY, MZ, CSGZ, BMOM, RATE, DVOL, FLOW, HEAT, HBOT, HTOP, AMPS or CHRG, FLUX, CURT, VLTG Nodal reaction forces in the nodal coordinate system. The reaction forces returned are the total forces: static, plus damping, plus inertial, as appropriate based on analysis type (see PRRSOL command). The first exception is modal analyses and mode-superposition transient analyses where static forces are returned. The second exception is spectrum analyses where the PRRFOR logic is used internally. In this case, the reaction forces are based on the type of force requested (using ForceType with combination commands, such as SRSS, PSDCOM, etc.). The third exception is reaction forces at a node attached to a SHELL294 element where HBOT and HTOP are always evaluated using the PRRFOR logic internally.

ORBT

A, B, PSI, PHI, YMAX, ZMAX, Whirl

Whirl orbit characteristics:

A is the semi-major axis.

B is the semi-minor axis.

PSI is the angle between the local axis y and the major axis Y.

PHI is the angle between initial position (t = 0) and major axis.

YMAX is the maximum displacement along local y axis.

ZMAX is the maximum displacement along local z axis.

Whirl is the direction of an orbital motion (-1 is backward whirl, 1 is forward whirl, and 0 is undetermined).

Angles PSI and PHI are in degrees and within the range of -180 through +180.

Orbits are available only after issuing a PRORB command.

Note: Use this command carefully when N represents an internal node, as the nodal degrees of freedom may have different physical meanings.

`Entity` = `NODE`, `ENTNUM` = `N` (node number) for averaged nodal results based on selected elements:
GET, `Par`, NODE, `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description	Item2
S	X, Y, Z, XY, YZ, XZ	Component stress.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
	1, 2, 3	Principal stress.
	INT, EQV	Stress intensity or equivalent stress.
	MAXF	Maximum stress failure criterion.
	TWSI	Tsai-Wu strength failure criterion.
	TWSR	Inverse of Tsai-Wu strength ratio index failure criterion.
EPTO	X, Y, Z, XY, YZ, XZ,	Component total strain (EPEL + EPPL + EPCR).
	1, 2, 3	Principal total strain.
	INT, EQV	Total strain intensity or total equivalent strain.
EPEL	X, Y, Z, XY, YZ, XZ	Component elastic strain.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
	1, 2, 3	Principal elastic strain.
	INT, EQV	Elastic strain intensity or elastic equivalent strain.
	MAXF	Maximum strain failure criterion.
EPPL	X, Y, Z, XY, YZ, XZ	Component plastic strain.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
	1, 2, 3	Principal plastic strain.
	INT, EQV	Plastic strain intensity or plastic equivalent strain.
EPCR	X, Y, Z, XY, YZ, XZ	Component creep strain.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
	1, 2, 3	Principal creep strain.
	INT, EQV	Creep strain intensity or creep equivalent strain.
ESIG	X, Y, Z, XY, YZ, XZ	Components of Biot’s effective stress.
	1, 2, 3	Principal stresses of Biot’s effective stress.
	INT	Stress intensity of Biot’s effective stress.
	EQV	Equivalent stress of Biot’s effective stress.
CDM	DMG	Damage variable
CDM	LM	Maximum previous strain energy for virgin material
GKS	X, XY, XZ	Gasket component stress.
GKD	X, XY, XZ	Gasket component total closure.
GKDI	X, XY, XZ	Gasket component total inelastic closure.
GKTH	X, XY, XZ	Gasket component thermal closure.
EPTH	X, Y, Z, XY, YZ, XZ	Component thermal strain.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
	1, 2, 3	Principal thermal strain.
	INT, EQV	Thermal strain intensity or thermal equivalent strain.
EPSW		Swelling strain.	`Item2` controls whether nodal-averaged results are used. Valid labels are: AUTO - Use nodal-averaged results, if available. Otherwise use element-based results. ESOL- Use element-based results only. NAR - Use nodal-averaged results only.
FAIL	MAX	Maximum of all failure criterion defined for this node.
	EMAX	Maximum Strain failure criterion.
	SMAX	Maximum Stress failure criterion.
	TWSI	Tsai-Wu Failure Criterion Strength Index failure criterion.
	TWSR	Inverse of Tsai-Wu Strength Ratio Index failure criterion.
	USR1, USR2, ..., USR9	User-defined failure criteria.
	HFIB	Hashin Fiber Failure Criterion.
	HMAT	Hashin Matrix Failure Criterion.
	PFIB	Puck Fiber Failure Criterion.
	PMAT	Puck Matrix Failure Criterion.
	L3FB	LaRc03 Fiber Failure Criterion.
	L3MT	LaRc03 Matrix Failure Criterion.
	L4FB	LaRc04 Fiber Failure Criterion.
	L4MT	LaRc04 Matrix Failure Criterion.
NL	SEPL	Equivalent stress (from stress-strain curve).
	SRAT	Stress state ratio.
	HPRES	Hydrostatic pressure.
	EPEQ	Accumulated equivalent plastic strain.
	CREQ	Accumulated equivalent creep strain.
	PSV	Plastic state variable or plastic work/volume.
	PLWK	Plastic work/volume.
TG	X, Y, Z, SUM	Component thermal gradient and sum. Note: IT1NUM = SUM is not supported for coupled pore-pressure-thermal (CPT`nnn`) elements.
TF	X, Y, Z, SUM	Component thermal flux and sum. Note: IT1NUM = SUM is not supported for coupled pore-pressure-thermal (CPT`nnn`) elements.
PG	X, Y, Z, SUM	Component pressure gradient and sum.
EF	X, Y, Z, SUM	Component electric field and sum.
D	X, Y, Z, SUM	Component electric flux density and sum.
H	X, Y, Z, SUM	Component magnetic field intensity and sum.
B	X, Y, Z, SUM	Component magnetic flux density and sum.
CG	X, Y, Z, SUM	Component concentration gradient or vector sum.
DF	X, Y, Z, SUM	Component diffusion flux density or vector sum.
FMAG	X, Y, Z, SUM	Component electromagnetic force and sum.
HS	X, Y, Z	Component magnetic field intensity from current sources (in the global Cartesian coordinate system).
BFE	TEMP	Body temperatures (calculated from applied temperatures) as used in solution.
FICT	TEMP	Fictive temperature.
CAP	C0,X0,K0,ZONE, DPLS,VPLS	Material cap plasticity model only: Cohesion; hydrostatic compaction yielding stress; I1 at the transition point at which the shear and compaction envelopes intersect; zone = 0: elastic state, zone = 1: compaction zone, zone = 2: shear zone, zone = 3: expansion zone; effective deviatoric plastic strain; volume plastic strain.
FFLX	X, Y, Z	Fluid flow flux in poromechanics.
FGRA	X, Y, Z	Fluid pore pressure gradient in poromechanics.
PMSV	VRAT, PPRE, DSAT, RPER	Void volume ratio, pore pressure, degree of saturation, and relative permeability for coupled pore-pressure CPT elements.
MPDP	TOTA, TENS, COMP, RW	Microplane homogenized total, tension, and compression damages (TOTA, TENS, COMP), and split weight factor (RW).
EPFR		Free strain in porous media
DAMAGE	1,2,3,MAX	Damage in directions 1, 2, 3 (1, 2, 3) and the maximum damage (MAX).
GDMG		Damage
IDIS		Structural-thermal dissipation rate
CONT	STAT	Contact status.
	PENE	Contact penetration.
	PRES	Contact pressure.
	SFRIC	Contact friction stress.
	STOT	Contact total stress (pressure plus friction).
	SLIDE	Contact sliding distance.
	GAP	Contact gap distance.
	FLUX	Total heat flux at contact surface.
	CNOS	Total number of contact status changes during substep.
	FPRS	Actual applied fluid penetration pressure.
SRES	SVAR`n`	Selected result `n`th state variable.
	FLDUF0`n`	The `n`th user-defined field variable.
Element nodal results are the average nodal value of the selected elements.

Table 167: *GET Postprocessing Items, Entity = PATH

Entity = PATH, `ENTNUM` = 0 (or blank)
GET, `Par`, PATH, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
MAX	`Lab`	Maximum value of path item `Lab` from last path operation. Valid labels are the user-defined labels on the PDEF or PCALC command.
MAXPATH		Returns the maximum path number defined.
MIN	`Lab`	Minimum value of path item `Lab` from last path operation. Valid labels are the user-defined labels on the PDEF or PCALC command.
LAST	`Lab`	Last value of path item `Lab` from last path operation. Valid labels are the user-defined labels on the PDEF or PCALC command.
NODE		Value providing the number of nodes defining the path referenced in the last path operation.
ITEM	`Lab`	*`Item2`* = PATHPT, *`IT2NUM`* = n The value of `Lab` at the `n`th data point from the last path operation.
POINT	`n`	*`Item2`* = X,Y,Z, or CSYS. Returns information about the nth point on the current path.
NVAL		The number of path data points (the length of the data table) from the last path operation.
SET	`n`	*`Item2`* = NAME. Returns the name of the nth data set on the current path.
NUMPATH		Returns the number of paths defined.

`Entity` = PATH, `ENTNUM` = n (path number)
Item1	IT1NUM	Description
`NAME`		Returns the name of the nth path.

Table 168: *GET Postprocessing Items, Entity = PLNSOL

`Entity` = PLNSOL^[a], `ENTNUM` = 0 (or blank)
GET, `Par`, PLNSOL, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
MAX		Maximum value of item in last contour display (PLNSOL, PLESOL).
MIN		Minimum value of item in last contour display (PLNSOL, PLESOL).
BMAX		Maximum bound value of item in last contour display (PLNSOL, PLESOL).
BMIN		Minimum bound value of item in last contour display (PLNSOL, PLESOL).

^[a]You must issue the /SHOW command before commands that produce a graphical output when running in batch mode to produce/export graphic files. For more details, see External Graphics Options in the Basic Analysis Guide.

Table 169: *GET Postprocessing Items, Entity = PRENERGY

Note: Available after the PRENERGY command is issued. `Entity` = PRENERGY, `ENTNUM` = `N` (component number)
GET, `Par`, PRENERGY, `N`, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
NCMP		Number of components (`ENTNUM` not required). This value is the maximum value for `N`.
NENE		Number of energy types (`ENTNUM` not required). This value is the maximum value for `M`.
TOTE	`M`	Total energy of type `M` of the model (`ENTNUM` not required). Energy value is non-zero when `Cname1` is blank on prior PRENERGY command.
ENG	`M`	Energy of type `M` of component `N`. Energy value is non-zero when `Cname1` is specified on prior PRENERGY command.
PENG	`M`	Percentage of energy of type `M` of component `N`. Percentage of energy value is non-zero when `Cname1` is specified on prior PRENERGY command.
Ordering of `N` and `M` corresponds to PRENERGY output.

Table 170: *GET Postprocessing Items, Entity = PRERR

`Entity` = PRERR, `ENTNUM` = 0 (or blank)
GET, `Par`, PRERR, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
SEPC[1]		Structural percent error in energy norm (PRERR).
TEPC[1]		Thermal percent error in energy norm (PRERR).
SERSM[1]		Structural error energy summation (PRERR).
TERSM[1]		Thermal error energy summation (PRERR).
SENSM[1]		Structural energy summation (PRERR).
TENSM[1]		Thermal energy summation (PRERR).

Some element- and material-type limitations apply. For more information, see the documentation for the PRERR command.

Table 171: *GET Postprocessing Items, Entity = RAD

`Entity` = RAD, ENTNUM = 0 (or blank)
GET, `Par`, RAD, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
VFAVG		Value of the average view factor computed from the previous VFQUERY command.

`Entity` = RAD, ENTNUM = n (enclosure number)
GET, `Par`, RAD, `n`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NETHF		Value of the net heat flux lost by an enclosure. For a perfect enclosure, it should be zero (due to numerical roundoff, it may be a small number close to zero). For an imperfect enclosure, it is the net heat escaping from the enclosure to the space node.

Table 172: *GET Postprocessing Items, Entity = RSTMAC

Note: Available after RSTMAC command is issued. `Entity` = RSTMAC, `ENTNUM`= `N` (solution number on `File1`)
GET, `Par`, RSTMAC, 0 or `N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NS1		Total number of solutions (modes for example) read on `File1`. See `Sbstep1` on the RSTMAC command. This value is the maximum value for `N`.
NS2		Total number of solutions (modes for example) read on `File2`. See `Sbstep2` on the RSTMAC command. This value is the maximum value for `M`
MAC	M	Modal assurance criterion value (MAC) between the solution `N` read on `File1` and the solution `M` read on `File2`. Note: `N` and `M` do not correspond to the substep (or mode) numbers if NS1 and NS2 are different from the total number of substeps (or modes).
MACCYC	M	Modal assurance criterion value (MAC) from compressed table for CYCLIC between the solution `N` read on `File1` and the solution `M` read on `File2`. Note: `N` and `M` do not correspond to the substep (or mode) numbers if NS1 and NS2 are different from the total number of substeps (or modes).

Table 173: *GET Postprocessing Items, Entity = SECR

`Entity` = SECR,`ENTNUM` = `n` (element number) For beam and pipe (including elbow) section results, return values for all elements if the element number (`n`) is blank or ALL.
GET, `Par`, SECR, n, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description	Item2	IT2NUM
S	X, Y, Z, XY, YZ, XZ	Component total stress	MAX – Returns maximum MIN – Returns minimum MAXY – Returns section Y location of maximum MAXZ – Returns section Z location of maximum MINY – Returns section Y location of minimum MINZ – Returns section Z location of minimum IVAL – Returns value at section node or integration point at element I node JVAL – Returns value at section node or integration point at element J node KVAL – Returns value at section integration point at element K node (ELBOW290) --- For IVAL, JVAL, and KVAL: The ALL (or blank) option for the element number is not valid. A specified element (n) is required.	These values apply only when Item2 = IVAL, JVAL, or KVAL. --- For beam and pipe elements: This value is the RST section-node number when KEYOPT(15) = 0. This value is the integration-point number when KEYOPT(15) = 1. For the ELBOW290 element: This value is the selected section- integration-station number. --- The numbers can be visualized via SECPLOT, ,6.
	1, 2, 3	Principal stress value
	INT	Stress intensity value
	EQV	Equivalent stress value
EPTO	X, Y, Z, XY, YZ, XZ	Component total strain
	1, 2, 3	Principal total strain value
	INT	Total strain intensity value
	EQV	Equivalent total strain value
EPEL	X, Y, Z, XY, YZ, XZ	Component elastic strain
	1, 2, 3	Principal elastic strain value
	INT	Elastic strain intensity value
	EQV	Equivalent elastic strain value
EPTH	X, Y, Z, XY, YZ, XZ	Component thermal strain
	1, 2, 3	Principal thermal strain value
	INT	Thermal strain intensity value
	EQV	Equivalent thermal strain value
EPPL	X, Y, Z, XY, YZ, XZ	Component plastic strain
	1, 2, 3	Principal plastic strain value
	INT	Plastic strain intensity value
	EQV	Equivalent plastic strain value
EPCR	X, Y, Z, XY, YZ, XZ	Component creep strain
	1, 2, 3	Principal component creep strain value
	INT	Component creep strain intensity value
	EQV	Equivalent component creep strain value
EPTT	X, Y, Z, XY, YZ, XZ	Component total mechanical and thermal and swelling strain
	1, 2, 3	Principal total mechanical and thermal and swelling strain value
	INT	Total mechanical and thermal and swelling strain intensity value
	EQV	Equivalent total mechanical and thermal and swelling strain value
EPDI	X, Y, Z, XY, YZ, XZ	Component diffusion strain
	1, 2, 3	Principal diffusion strain value
	INT	Diffusion strain intensity value
	EQV	Equivalent diffusion strain value
NL	SEPL	Plastic yield stress
	SRAT	Plastic yielding (1 = actively yielding, 0 = not yielding)
	HPRES	Hydrostatic pressure
	EPEQ	Accumulated equivalent plastic strain
	CREQ	Accumulated equivalent creep strain
	PLWK	Plastic work/volume
YSIDX	TENS,SHEA	Yield surface activity status: 1 for yielded and 0 for not yielded.
FPIDX	TF01,SF01, TF02,SF02, TF03,SF03, TF04,SF04	Failure plane surface activity status: 1 for yielded and 0 for not yielded. Tension and Shear failure status are available for all four sets of failure planes.

Table 174: *GET Postprocessing Items, Entity = SECTION

`Entity` = SECTION,`ENTNUM` = `component` (listed below). Generate data for section stress results, using PRSECT before retrieving these items. Valid labels for `ENTNUM` are MEMBRANE, BENDING, SUM (Membrane+Bending) , PEAK, and TOTAL. (The following items are not stored in the database and the values returned reflect the last quantities generated by PRSECT or PLSECT.) Only MEMBRANE, BENDING, and SUM data are available after a PLSECT command. The MEMBRANE label is only valid with `Item1` = INSIDE.
GET, `Par`, SECTION, `component`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Item2	Description
INSIDE	S	X, Y, Z, XY, YZ, XZ	Stress component at beginning of path.
		1, 2, 3	Principal stress at beginning of path.
		INT, EQV	Stress intensity or equivalent stress at beginning of path.
CENTER	S	X, Y, Z, XY, YZ, XZ	Stress component at midpoint of path.
		1, 2, 3	Principal stress at midpoint of path.
		INT, EQV	Stress intensity or equivalent stress at midpoint of path.
OUTSIDE	S	X, Y, Z, XY, YZ, XZ	Stress component at end of path.
		1, 2, 3	Principal stress at end of path.
		INT, EQV	Stress intensity or equivalent stress at end of path.

Table 175: *GET Postprocessing Items, Entity = SORT

`Entity` = SORT, `ENTNUM` = 0 (or blank)
GET, `Par`, SORT, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
MAX		Maximum value of last sorted item (NSORT or ESORT command).
MIN		Minimum value of last sorted item (NSORT or ESORT command).
IMAX		Node/Element number where maximum value occurs.
IMIN		Node/Element number where minimum value occurs.

Table 176: *GET Postprocessing Items, Entity = SSUM

`Entity` = SSUM, `ENTNUM` = 0 (or blank)
GET, `Par`, SSUM, 0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
ITEM	`Lab`	Value of item `Lab` from last SSUM command. Valid labels are the user-defined labels on the ETABLE command.

Table 177: *GET Postprocessing Items, Entity = VARI

`Entity` = VARI, `ENTNUM` = `N` (variable number after POST26 data storage) (for complex values, only the real part is returned with Item1 = EXTREM)
GET,`Par,VARI,N`, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
EXTREM	VMAX	Maximum extreme value.
	TMAX	Time or frequency corresponding to VMAX.
	VMIN	Minimum extreme value.
	TMIN	Time or frequency corresponding to VMIN.
	VLAST	Last value.
	TLAST	Time or frequency corresponding to VLAST.
	CVAR	Covariance
REAL	f	Real part of variable `N` at time or frequency f.
IMAG	f	Imaginary part of variable `N` at frequency f.
AMPL	f	Amplitude value of variable `N` at frequency f
PHASE	f	Phase angle value of variable `N` at frequency f
RSET	`Snum`	Real part of variable `N` at location `Snum`.
ISET	`Snum`	Imaginary part of variable `N` at location `Snum`.

`Entity` = VARI, `ENTNUM` = 0 (or blank) (after POST26 data storage)
GET,`Par`,VARI,0, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Description
NSETS		Number of data sets stored.

Table 178: *GET Postprocessing Items, Entity = XFEM

`Entity` = XFEM, `ENTNUM` = 0 (or blank)
GET, `Par`, XFEM, 0, `Item1`, `IT1NUM`*
Item1	IT1NUM	Description
STAT	`Element Number`	Status of the element: 0 = uncracked, 1 = cracked

Entity = XFEM, ENTNUM = NODE

*GET, Par, XFEM, NODE, Item1, IT1NUM, Item2, IT2NUM

Item1 IT1NUM Item2 IT2NUM Description

ELEM

Element Number

POS (or blank)

1-4 (for 2D elements)

1-8 (for SOLID185)

Node number at position IT2NUM of cracked element

`Entity` = XFEM, `ENTNUM` = PHI
GET, `Par`, XFEM, PHI, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Item2	IT2NUM	Description
ELEM	`Element Number`	NODE	`Node Number`	LSM Phi value for this node number of this element

`Entity` = XFEM, `ENTNUM` = PSI
GET, `Par`, XFEM, PSI, `Item1`, `IT1NUM`, `Item2`, `IT2NUM`*
Item1	IT1NUM	Item2	IT2NUM	Description
ELEM	`Element Number`	NODE	`Node Number`	LSM Psi value for this node number of this element

Menu Paths

Utility Menu>Parameters>Get Scalar Data